Snapping to reference points in sketching breaks
Hi @jamie.q.white,
Sorry to hear this has been happening to you! I saw some of your other posts recently, and hopefully we can try to avert some of the pain.
As far as this snapping issues goes, I have seen this before, but it has been tricky to recreate. For example, I don't think I have ever run into this issue personally, on my laptop. I have seen it on other customers computers, and unfortunately I did not keep track of whether or not it was a Mac or Windows (if that even matters). I just tried to recreate this issue multiple times on different designs of mine and could not.
A few things to check however - in your preferences, in the general-design tab, do you have Auto-Project geometry selected? Do you ever notice it toggling itself on/off?
Also, as a workaround to that issue, does going into the sketch menu and selecting Project and then selecting your cylinder allow you to snap to it? Or if you go into the Construct menu and select point at center of cylinder?
Thanks,
James Youmatz
Product Insights Specialist for Fusion 360, Simulation, Generative Design
Hi @Anonymous,
What is happening in that scenario is that when you window select and delete those entities, you are also in turn deleting the reference that is in place when you create the sketch on the face. (Notice how the yellow profile disappears). This is also the same behavior you would expect in Inventor for instance. In this instance, you will have to go and reproject the geometry back into the active sketch plane in order to snap to the reference geometry. This should work, can you confirm it does?
Thanks,
James Youmatz
Product Insights Specialist for Fusion 360, Simulation, Generative Design
I've actually turned the autprojection feature off in the preferences. I prefer control over convenience:
One thing I notice, @jamie.q.white, in your original video, is that I don't see the yellow profile that I would expect, once you have started the sketch for the cylinder:
What I would expect to see is more like this:
which makes me wonder: Is the sketch really located on the top of the cylinder? Or is it actually on the origin plane behind the cylinder? The cylinder in that video is so thin that it's hard to tell. That would explain why you cannot snap to the edges of the cylinder. I was able to get a similar effect if the thin cylinder was made unselectable. I didn't see any bodies or components in your model marked unselectable, though.
Can you try this workflow again with a thicker base cylinder, and see whether you get the shaded profile as above, and can clearly tell, by rotating the view, that the sketch is on the top face of the cylinder, and not behind it?
thanks,
Jeff Strater (Fusion development)
Jeff Strater
Engineering Director
Could you share your selection filter settings ?
I am noticing in the video that afte the selection of the sketch plane nothing on the cylinder highlights, whcih is VERY untypical for Fusion 360, where usually everything that could possibly be selected blinks and flickers to indicate it can be selected.
The only time I've seen this happeninng, as Jeff suggested is if either the component is set to "not selectabale", or I outsmarted myself and and forgot that previously I had change the selection filters, which can have a very similar effect.
Ah, good catch @michallach81! You are correct. This is the problem: The sketch folder is hidden, so you cannot see the sketch geometry, so you cannot snap to it! You can see this (it's a little hard to see because of the Screencast command history) in @jamie.q.white's original video:
The bug here is that there is no warning. If you just create a sketch in this state, you see this error:
but, because Cylinder uses a simplified form of the sketch environment, this warning does not appear. I will file this bug.
Jeff
Jeff Strater
Engineering Director
Exactly! That warning message is the reason I don't hide an entire sketches folder anymore.
Very good catch @michallach81 !
While this is certainly a bug, it generally points to a workflow issue!
You can turn of sketches to de-clutter your workspace.
You can also turn off sketch folders to de-clutter your workspace. You just have to turn them on when you want to start editing again.
The only bug is that there is no error message. That's an Fusion 360 issue.
Whether Fusion 360 warns you or not, you'll still have to turn the sketch folder back on. Has this stumped me a few times before ?
Sure, but I've learned and adjusted my workflow. That's why I called it a workflow issue.
A screencast would be helpful, thank you. I have not seen a case where you don't get the geometry inferences, but a case certainly could exist.
One small point: If you are doing fully parametric designs, I would recommend staying away from the primitives (cylinder, block). They do not update parametrically, especially for those geometry relations to the sketch. Here is a quick screencast showing this problem/behavior:
in this video, the second cylinder I create, though I created it tangent to the base cylinder, does not obey this if I edit the base:
The historical reason for this is primitives were first envisioned as just a quick way to play with geometry. They were not expected to be building blocks for more complex parametric designs. This behavior is a known problem, and we do plan to fix this.
However, in the meantime, I would recommend that you just use sketch + circle + extrude to make cylinders that you expect to be associative.
I realize that this is not the problem you are experiencing, but it will likely bite you further down the road, so I thought I'd warn you.
Jeff
Jeff Strater
Engineering Director